What Is Four Axis Machining?

• 1
  Key takeaways
• 2
  What is four axis machining and how the cut changes
• 3
  Setup rules that decide whether four axis machining holds tolerance
• 4
  Tolerances, surface finish and size limits
• 5
  Material behavior on a rotating table
• 6
  When four axis machining is the right call
• 7
  Four axis vs three axis vs five axis

A three-axis mill moves the tool in X, Y and Z. The workpiece stays still. To reach the back face you unclamp it, turn it, re-clamp it, and pick up the datum again. Every re-fixture costs time and adds a stack of position error that you cannot remove later.

Four axis machining adds a rotary table that turns the workpiece. On a vertical mill the axis is usually A, rotating about X. Mount the part on the table centerline and the same tool can reach four sides of a block without anyone touching the clamps.

The key mechanical difference is the distance from the rotary centerline to the cutting edge. That radius changes as the part turns, so the tool tip speed at the surface changes with it. Feed rates written for a flat face will run hot or slow on a turned diameter.

On our 12 four-axis mills the table is Ø400 mm and the machines hold ±0.005 mm on indexed features. That is the same tolerance class as our three-axis work, provided the part is dialed in within a few microns of the centerline.

• 1
  A axisRotation about X, the most common fourth axis on a vertical mill.
• 2
  B axisRotation about Y, common on horizontal mills and mill-turn centers.
• 3
  IndexedTable locks, then the cut runs; position repeats from the servo.
• 4
  ContinuousTable turns while cutting, used for wrapping a slot or a cam profile.

The rotary centerline is the datum for everything. If the part sits 0.05 mm off the true center, every feature cut at a different index inherits a position error of the same size or more, depending on the radius. Dial the stock in, not the finished face.

Workholding matters more than on a three-axis job. A three-jaw chuck on a round bar, a collet block for square stock, or a fixture plate with a tailstock all work. Long parts need the tailstock; unsupported overhang flexes and the surface finish goes first, then the size.

Tool length and reach set the limit on how deep you can go around a diameter. A long end mill in a deep cavity will chatter before the axis runs out of travel. Short tool, small stepover, and a light radial depth of cut usually beat a long tool pushed hard.

Program the rotation as a positioning move, then cut. Treat each face like a separate operation but without losing the datum. That habit keeps the CAM output readable and makes it easy to check the post-processor is outputting the right rotary direction.

• 1
  Dial to centerlineWithin a few microns on the diameter that drives the feature positions.
• 2
  Support long partsTailstock or steady rest; unsupported overhang kills finish and size.
• 3
  Keep tools shortReach sets the depth limit more often than machine travel does.
• 4
  Index, then cutPositioning moves are safe; verify rotary direction in the post.

Indexed four-axis work holds ±0.005 mm on features cut from the same setup, matching our three-axis capability. Angular position repeats well too, but the linear error at the feature grows with the radius from the centerline. A 0.01° error is nothing at 20 mm and visible at 200 mm.

Surface finish depends on the cut, not the axis count. As-machined aluminum lands around Ra 1.6–3.2 μm. Fine finishing with a small stepover gets Ra 0.8–1.6 μm, and lapping or polishing takes it to Ra 0.2–0.8 μm where the geometry allows.

Continuous rotary cutting, where the table turns under the tool, is a different animal. Feed is programmed in degrees per minute at the surface, and the effective chip load changes with radius. A wrapped slot on a Ø60 mm boss needs a different feed from the same slot on a Ø200 mm flange.

Size is bounded by the machine, not the concept. Our four-axis mills take parts up to the Ø400 mm rotary table, and our larger travels reach 4,000 × 400 × 150 mm on the long-axis machines for shaft-type work. Beyond that the part moves to a mill-turn center or a five-axis machine.

• 1
  Indexed accuracy±0.005 mm on features cut in one setup.
• 2
  Angular errorMultiplies by radius; check the outermost feature, not the bore.
• 3
  Finish rangeRa 3.2 μm as-machined down to Ra 0.2 μm polished.
• 4
  SizeØ400 mm rotary table; long shafts up to 4,000 mm on larger travels.

Aluminum 6061 and 7075 cut cleanly on a fourth axis. They are light, so the rotary servo is not fighting much inertia, and index times stay short. 7075 holds a better finish on thin walls but is less forgiving of a dull tool.

Stainless 304 and 17-4PH work well for shafts, valve bodies and fittings. They work-harden, so keep the feed up and never let the tool rub. Continuous rotary cutting on stainless is where a rigid setup shows its value; chatter appears fast on a long, unsupported diameter.

Titanium and Inconel raise the heat. Coolant through the tool helps, and the rotary table should index while the tool is clear of the cut. Pulling a cutter out of a deep titanium pocket with the table turning is a good way to break an edge.

Plastics like POM, PEEK and ABS machine easily but move with temperature. On a long part, the heat from cutting can grow the stock enough to shift the feature positions between indexes. Rough, cool, then finish.

• 1
  AluminumFast indexing, good finish, low inertia on the rotary servo.
• 2
  StainlessKeep feed up; work-hardening punishes a rubbing tool.
• 3
  TitaniumIndex clear of the cut; manage heat with through-tool coolant.
• 4
  PlasticsRough and cool before finishing to control thermal growth.

Pick four axes when the features wrap around one centerline. A hydraulic manifold with ports on four faces, a camshaft with lobes at set angles, a sensor housing with connectors on three sides. These parts want one setup and one datum.

Pick three axes when the part is a plate. If every feature is reachable from the top, adding a rotary table only adds setup time and a new error source. Two-sided plates are often faster as two three-axis operations than as one four-axis job.

Pick five axes when the surface is freeform or the tool has to lean to clear a wall. Impellers, turbine blades and deep pockets with undercuts need the tool vector to change while cutting. Four axes cannot tilt the tool into a corner.

The cost signal is simple. Four-axis work removes a re-fixture and one datum transfer. If your part needs three or more setups on a three-axis machine, the fourth axis usually pays for itself on the first run.

• 1
  Choose 4-axisFeatures on several faces around one centerline, long shafts, cams.
• 2
  Choose 3-axisPlate-like parts cut from the top in one or two setups.
• 3
  Choose 5-axisFreeform surfaces, undercuts, tool clearance in deep pockets.
• 4
  Cost ruleThree or more re-fixtures on a 3-axis machine favors 4-axis.